Official Luthiers Forum!

Anyone have experience with either RhinoCAM or VisualMill?

Mecsoft's site is pretty confusing saying features are available in the basic version in one area and not available in another area.

I'd like to be able to manually tweak toolpaths if need be. As far as I can tell that's only available in the Pro version.

What about containment boundries around objects when 3D machining? Available in basic?


Backplotting possible?

Hey Sheldon, I use RhinoCAM in my home shop. You can easily establish containment boundaries in RhinoCAM basic by selecting the containment geometry before starting the 3d toolpath function.

I use RhinoCAM basic and have found it to be adequate for basic carving operations. For simpler things like inlay, it works fine as well.

I believe VM and RC are sister products...one is integrated into Rhino while the other is not...

_________________
http://www.PeakeGuitars.com

Thanks Parser. That was my biggest concern.

I see a lot of features in the Pro version that would be very useful, but I can't justify the $4K. From what I can tell though, the machine between two curves would be the best way to machine a neck shaft.


How do you handle edge roundovers? The basic version doesn't include that bit profile. I suppose you could do a profile cut and limit the depth to the radius of the bit.

Hey Sheldon, for most electric & bass necks you can just use a parrallel toolpath for carving.

For acoustic necks, you typically have to take a bit of a different approach due to the height of the heel. I machine them as two separate areas. I machine the heel area first...and then I machine the shank. For the heel, I use a horizontal roughing toolpath (if I remember correctly!). For the shank, I use a parrallel toolpath as I would on an electric neck.

For running a roundover bit along the profile of an electric body, You can get away with setting up a toolpath to cut the contour of the part and then offset it in the appropriate distance for the bit you are using. It's very simple to do and works great...no worries! The only tricky part of this is if you are rounding over geometry that is not flat. In this case, you have to take care not to allow the edge of the bit to bite into any upwardly sloping surfaces...a belly carve is a good example of this. It's better to take too little material than too much in this situation!

_________________
http://www.PeakeGuitars.com

Thanks Parser.

Doesn't parallel finishing leave pretty large scallops on the edges of the neck shaft? I haven't used that strategy in a long time, but that is my memory of it. Maybe follow up with horizontal finishing to clean up the edges?

The tool paths I use now taper in relation to the shaft taper. I'm not sure what this strategy is called, but I really like the results.

Hey Sheldon - it is all about how you set your stepover. If you use a .125" stepover and a 1/2" ball mill you will have some cleanup work to do. but if you use a small enough stepover then you should be able to get things carved to an appropriate level (keep decrease the stepover until you get good results). Keep in mind that on necks, parallel finishing works particularly well because the neck itself is a linear shape. Parallel finishing does not work quite as well on carved bodies & things like that....for that stuff it is beneficial to use a toolpath that follows the contours of the part.

_________________
http://www.PeakeGuitars.com

I'd assume you're talking about a flowline toolpath, Sheldon. Those stepover on the surface rather than on an axis, so you don't need to overcompensate for the edges of the neck by making the stepover super small all over.

On many parts, you need to use multiple toolpaths. A carved top guitar is the perfect example as you WILL want to use a parallel finishing path on the top, but a contour (aka : horizontal) path on the sides. Depending on how well a neck was designed for machining, I end up using between one and four paths on the back of a neck.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

That sounds about right. The stepover is a percentage of the surface. What I like about it is that the shaft is machined with straight lines. There's no wasted movement. A typical neck carve file is less than 10K. What I don't like about it is that it's only good for simple contours like the shaft. It can't do the blends at the headstock and heel.



If you don't mind me asking, what is the best path to avoid grain blowout on the treble side of the heel and bass side of the head where the rotation of the cutter is working against you?

In my experience, it is more beneficial on a carved top guitar to have a toolpath that follows the contours of the body.
It is possible to use a parallel finishing type toolpath...but the stepover required to get an adequate finish would be smaller than the stepover required to get an adequate finishing using the other method. The one drawback is that you need something more powerful than RhinoCAM basic in order to write this type of toolpath. MasterCAM works well, and it should, at roughly 10X the cost. I have not had a chance to use the professional version of RhinoCAM. Another drawback to using a parallel toolpath is that the scallops between the toolpaths will be all along the edge of the part. Sanding seems to be easier if these scallops follow the topography more closely. Another thing to keep in mind is that you should not approach wood machining as you would metal. In metalworking, a closer stepover is generally equated with an improved part. In woodworking, you reach a point where you are just running the machine longer than you need to...once you get the peak heights to a certain point they sand off very easily.

As for chip-out, there are a few basic things you can check to get this in line. First is the feed & speed combination for your program. If you are running too slow of a spindle speed for a given feed rate, this can lead to chip out. It will appear first in certain trouble spots and then get worse as the conditions move further from optimum. Another cause is tool wear. If the edges aren't good and sharp, it will tear the grain instead of shearing it cleanly. Another good preventative measure is to make sure you are using a climb cut, which means that you should be moving in a clockwise motion around the part. Finally, if your depth of cut is excessive, this can also aggravate the situation.

I'm not sure I understand how this is different from Horizontal Finishing, but it probably has something to do with the Z being able to move along the contour as well.

The more I look into it, the more I think that the Pro version is what's needed.

Re-read my post; it uses two toolpaths. The perceived 'choice' that needs to be made only exists if you try to machine the entire part with one toolpath, and we don't do it that way for the exact reasons you brought up. Horizontal contoured surfaces which are relatively flat machine best with a parallel toolpath and vertical walled surfaces machine best with a vertical stepdown.

There are some really good ways to avoid chipout without sacrificing speed on the toolpath side, but I'll have to file those under trade secrets. A lot of innocent wood suffered (along with my wallet) so that I could cut more of it faster. In general you'll get less chipout with climb cuts, higher RPM, and smaller cutters (and, of course, sharper cutters). You can substitute more flutes for higher RPM in the right situation, but there are forces at work that put a floor on the RPM a certain wood will cut well at regardless of the number of flutes.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

For clarity, the toolpaths I'm talking about:

Parallel : Machines either in XZ or YZ plane and steps over in the third axis (ie: each pass has a constant X or Y value, whichever is the stepover)

Contour : Machines in the XY plane and steps over in the Z (also called Z level and horizontal)

They're both types of parallel toolpaths in that each pass is on a plane parallel to the one before it.

Also, as a quick tip, if you're using a parallel toolpath then you'll want the stepover to be on your heaviest, slowest, or least rigid axis. So, if on a gantry style machine, you'll get best results stepping the gantry over (ie: only moving the gantry between passes).

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

I guess the overall moral is that you need to spend enough time experimenting with your software, your machine, and your fixtures to figure out what works best for you. Admittedly, I do things one way at work and another way at home (there is a big difference in the equipment I use in both those places!).

_________________
http://www.PeakeGuitars.com

Hope this isn't too far off topic, guys, but I have a question on ball nose cutters. I may have asked this here before (can't remember--getting old) but are there any thoughts on how to overcome the problem of zero surface speed at the center of a ball nose cutter? Tearout can be an issue at the center for this reason. It's really noticeable, when machining a contour, that the cutter does a great job when the surface being cut is slightly off 90 to the axis of the spindle and the contact point of the cutter is slightly off center.
I've considered mounting an auxiliary spindle at a slight angle, say 10 degrees, so that on a finishing pass the contact won't be on center of the cutter.

Good tip Bob, thanks. I'd never thought about that.

Nelson, that's a good question. My 2 cents is that lately I've started cutting convex profiles from the bottom up. The router works a little harder, but I feel it cuts down on the grunt work for the center of the bit. It seems to leave a slightly better finish and hopefully will keep the center section sharper longer.

With sufficient overlap, the ballnose actually cuts most of the stock on a pass away on the pass before it. IE: The 'tip' is never cutting into very much stock because the side already hit it last pass. If you're taking enough passes, then the tip compresses the wood more than cutting it on its way through. So, short answer is that the tip should never be cutting enough stock to make a mess of it.

The best illustration I've seen of both points is cutting a slot through a piece of ebony with a ball-nose. The bottom of the slot is really raggedy looking but the sides are shiny. Compare that, though, to a fingerboard which was cut with a bunch of passes, which is almost completely shiny. (Note that if you get your spindle speed up high enough the 'no stock to cut' effect works in a straight line and you can get a relatively shiny bottom on your channel.)

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Bob--The tip of the cutter will either compress and/or tear the wood. In highly flamed maple it's, unfortunately, tearing. I see the probably mostly in cutting archtop plates particularly when the surface being cut is perpendicular to the cutter axis. I would love to see compression and that is the case more so in spruce.
It's interesting in that the cut cleans up beautifully when the cutter is in a sloped area such as the lower to upper bout transition. This is my logic behind tilting the axis of the spindle enough that at no time will the surface be perpendicular to the cutter axis. This would get away from the compression or tearing that occurs at the centerline of the cutter.
The tearing is no problem when doing the rough cuts, it's the finish pass before sanding that I would like to improve.

Highly figured woods will almost always show some tear out on a carve operation. I wouldn't recommend spending too much time trying to design an angled cutting head, figuring out how to program it, etc...on a carved top you will basically just be moving the problem from one area to another.

The best thing you can do for all of this is to get good cutters. Onsrud makes nices tools..

_________________
http://www.PeakeGuitars.com

Speaking of cutters, does anyone know of a ball mill with down shear? Hugh MacFarlain had one, but I can't remember if it was custom or not.

Nelson, PRS used to use a custom duplicarver and the head was tilted.

Just thinking out loud here. What about using a flat bottomed cutter with a corner radius? You would'nt be able to cut any concave surfaces, but the horizontalish surfaces would be beautiful.

My thought on a tilted spindle would be mounting to the existing spindle nose with an adapter off to one side. The exact center of the cutter ball would fall on the same center as if it were mounted in the vertical spindle. The angled spindle would be very small and high speed but use the same program as the vertical roughing spindle. Probably would use a carbide burr type ball for the finish cut since it would only be taking off a few thou. The angle would probably be at least 30 degrees to vertical, maybe 45, so that the cutter is never touching at it's centerline.

Sheldon--I'll bet there are some downshear ball nose out there. I'll keep the eyes open. Interesting about PRS.

That's what I said (well, I called it cutting; tearing is cutting where the edge wasn't keen enough to push through). The goal is to turn it all into compression rather than tearing. If you've got the right RPM and a sharp cutter then it's just a matter of smooth tool motion and the proper toolpath.

In terms of chipout, the issue is how much force is being put on the part when machining. If the cutter's putting more stress on the part than it's cohesiveness then you get pieces flying off. Taking this into account when toolpathing allows you to avoid it, though sometimes you need to use some pretty nonstandard techniques.

RobbJack will make a left spiral ballnose for you, I'm sure. They make nice stuff and the pricing is good considering the product.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

Bob

Wasn't sure what you meant by this:

(Note that if you get your spindle speed up high enough the 'no stock to cut' effect works in a straight line and you can get a relatively shiny bottom on your channel.)

I do run 25K RPM and in the area of 100 IPM to 220 IPM when contouring with a 3/4" dia. ballnose. This is a two flute brazed carbide zero rake cutter. (about $15 ea.) I'm sure there are better choices out there. Any suggestions?

Nelson

I meant that if your speed is high enough or your feed is low enough then the cutter will have cut nearly all the stock from a particular point before the low-velocity edges hit, and thus the finish can still be good as it's only compressing a half thou of stock or somesuch.

RobbJack makes good cutters, as does OSG. The cutters companies make especially for aluminum have sharper edges than regular end mills and they cut wood better. That said, the standard flat and ballnose end mills work just fine.

_________________
Bob Garrish
Former Canonized Purveyor of Fine CNC Luthier Services

I haven't found any difference in the quality of cut between HSS and good quality carbide, but everything I've read says there is. What's been your experience guys?

In my experience, HSS seems to be to the better choice. I believe carbide cutters are made for cutting harder materials, and they have a more blunt edge. HSS is adequate hardness for cutting wood and seems to work fine. You should get pretty decent life out of HSS tools.

For wood I do prefer a shallower helix angle than aluminum cutting tools typically have.

_________________
http://www.PeakeGuitars.com